I am using the interFoam-solver. Alpha1 is characterizing the volume fraction (alpha1= 0 means: there is only gas in the cell, alpha1=1 means: there is only liquid in the cell).
Now I´ve got the problem, that alpha1 is getting negative or greater than 1 which is not realistic.

My idea is to "correct" the alpha1 after every time step.
I need something which goes into every cell: If alpha1 is negative or nearly 0 (for example 0.1e-6), alpha1 should be put to 0. If alpha1 is greater than or nearly 1, alpha1 should be put to 1.

I would not suggest doing this, as MULES handles itself the boundedness, continuity and conservation of alpha1. Although you may obtain vales slightly lower than 0 or larger than 1, if your BCs are correctly set, these will only be on the order of machine precision.

I am using interFoam/waveFoam as well. I remember in the code, the value of alpha1 is restricted between 0 and 1. However, the case I am running at the moment gives out results like this, where Max(alpha1) = 1.57337. But the case is still running even though.

2. You are only solving the pressure equation one (1) time per time step.

If you relate that with the fact that interFoam/waveFoam is based on a PIMPLE-algorithm, then you will have no chance what so ever in obtaining mass conservation on the cell level; in your case the error in mass conservation is considerable. This is most probably the reason for the unboundedness of alpha1.

So: start solving for the momentum equation and have 3-4 iterations in the pressure equation per time step. This will greatly improve on your mass conservation problems and therefore improve on the boundedness of alpha1.

That's quite inspiring really. I'll resort to the code to work it out. By the way, I am using OF 1.7.1 based on PISO algorithm. However, in the cases I ran earlier, I didn't see alpha1 could be larger than 1.5, at most 1.0*.

the discussion is really helpful for me and I have got one question to it.

My simulations are not running very well. Soon after the beginning the velocities are increasing and as a result my time step is decreasing till the simulation stopps ( I am using adjustableRunTime). The turbulent viscosity is getting very small too.
I am using the k-epsilon-model.
At the beginning I thought that alpha1 is the reason for this behaviour but the discussion here gives some hints that the problem could be somewhere else.

Is there a possiblity to change something in the fvSolution-file so that the simulation get stable?

My suggestion is only meant for debugging. Turning off the turbulence, you can lower the complexity and see, whether the turbulence model is the cause of your problems. If yes, you know that you need to change e.g. the boundary conditions to stabilise the model.

You could also try to use upwind on all of the divergence schemes in fvSchemes.